Standard Parts Library: Configurations or Individual Parts?

[martin]

We are about to set up a new library and have been debating whether it is best to use configurations or individual part files for things like fasteners.

Here's my main concerns:

• Assembly performance, where upwards of a thousand fasteners could be used (but maybe only 5-10 different types)

• Effort in terms of library management and using it

• It needs to play nice with SOLIDWORKS PDM

---

I like the idea of just having one part file per ISO or DIN standard with configurations for all sizes and materials. Then we would have one entry point for making modifications if (when) we need to modify things like custom properties or add sizes, and use configuration publisher to allow the designer to pick the right config. I see the downside of using just one part if it is continuously modified as it will affect all the "where used" assemblies, but that shouldn't be that much of an issue if we include all possible variants from the start.

My main issue with individual parts is that will need to generate a hundreds if not thousands of additional files, and if we ever need to edit something it will be a lot of work and open up for more mistakes and inconsistencies. Browsing through the library to find something would also be less efficient. But it does seem like the safer (but more boring) option, since by having one file per part number / item in PDM and other systems we may avoid some challenges.

I haven't really considered Toolbox as it seems complicated to add custom hardware and I would hate to have some fasteners there and some in another library. I probed around in the SQLite database once (see attachment) to try figure out what was going on. Would be nice to know if anyone has experience with adding custom hardware and managing it over time.

[Frederick_Law]

Depends.
Will the part change?
"Library" part don't change. Like all standard nut and bolt.

Do you share SW files with supplier/customer?
One part one config is small file. Easy to send. Only part used will be send.
One part 1000000000 config is a huge file. Not easy to send. If you 100 of different parts with 1000000000 config, what will be the file size?
Toolbox could be big database file but only need to send when updated.

Similar with PDM.

[martin]

Depends.
Will the part change?
"Library" part don't change. Like all standard nut and bolt.

Do you share SW files with supplier/customer?
One part one config is small file. Easy to send. Only part used will be send.
One part 1000000000 config is a huge file. Not easy to send. If you 100 of different parts with 1000000000 config, what will be the file size?
Toolbox could be big database file but only need to send when updated.

Similar with PDM.

I agree they shouldn't really change. I'm mentioning this since we are doing a lot of other related work to align things like BOM templates and custom properties which mean we would have to update them to fix metadata. But probably better to get that work completed before doing any work on the new library parts...

We don't send native SOLIDWORKS files to any of our suppliers, we usually just send exported STEP files for manufacturing, so this shouldn't really matter much.

Realistically I doubt we would exceed 1000 configuration per part, most would probably be in the 10-200 range, but that's probably still a huge file compared to a single config part. We have certain sizes and materials we never use for example, so we don't need to add all variants defined by the standards.

[Frederick_Law]

Do some test.
Make file with 100 or 1000 config and see how big the files and if it's slow in assembly.

[Pernils]

Stay away from configurations if you want to help the downstream process.

My experience that you just can't by a screw that will somehow change length and dimension when you want to start to use it.
In MPS system every item in a structure needs a unique identity to be purchased and so on.

Configuration can at first glans seems to be a clever way to get around a problem but it will generate problems in other departments and situations.

[zwei]

I am interested on this too...

My personal preference is either
Part with single configuration OR Part with multiple configuration driven by design table

Avoid toolbox whenever possible, not to mention standard license does not support toolbox

I had heard good and bad thing about Part with multiple configuration so is a bit on the fence on this.

I dont really play with it a lot but...
Cadbooster fastener library does look like a decent library https://cadbooster.com/fastener-models/
Their lightning tool also seems quite interesting...

[bnemec]

If using PDM, and want to search for where used of the specific part, then don't use configs; actually I would say stick to the one part per file rule in that case.

Where used in PDM works pretty well, but not always. If you want to know the where used of a specific config in a file, you must first select the version of the file to select a specific config (standard part). Since the config file will likely get many versions as new parts/configs are added the where used will be across many versions, making the where used function in PDM worthless.

As Fred said, standard parts are never revised/changed and most likely do not have a part number in the ERP/MES/inventory system (or there is no system).

[martin]

I am interested on this too...

My personal preference is either
Part with single configuration OR Part with multiple configuration driven by design table

Avoid toolbox whenever possible, not to mention standard license does not support toolbox

I had heard good and bad thing about Part with multiple configuration so is a bit on the fence on this.

I dont really play with it a lot but...
Cadbooster fastener library does look like a decent library https://cadbooster.com/fastener-models/
Their lightning tool also seems quite interesting...

My current plan is to make parts with multiple configurations, and then save each configuration as a new part. If I need to fix something I can go back and do it from that one "template part" and save out the affected variants again, instead of having to go into each part and do the same.

Cadbooster's fastener models do look good. We require some additional ones, as well as we would need to configure custom properties for all of them. They do offer customization services for this which I am considering it. I'll probably do a trial on the lightning add-in to see how that works first, because it addresses one of my worries about having to browse through hundreds of files to find the right fastener.

The point about Toolbox licensing is valid, we have some professional and premium licenses, but a lot more standard licenses, so that could become a limitation.

[Glenn Schroeder]

Here's what I've been doing for a very long time. Each diameter bolt is a single Part file, with configurations for each length, and I didn't try to put in every length right away, but instead add them as needed. I have a configuration specific custom property linked to the length dimension, so whenever a new length is added the custom property is added also, and it's correct for the new configuration. I call out that property in the Drawing, in notes or BOM.

Similar to that, each nut size has its own Part file, with configurations for standard, heavy hex, coupling, etc, and washers have configurations for lock, F844, and F436.

I call out the grades for the bolts in the Drawing. Since I'm a one-man show that works fine. If you have one person doing the modeling and another doing the Drawing that might not work for you.

I would definitely not have a single file for all bolt sizes. That could turn into hundreds of configurations, and quickly become unmanagable.

You mentioned Assembly performance. By all means don't put threads on your hardware since that will greatly add to rebuild time. A few of my specialized bolts have threads so I can show them when I detail in a Drawing, but those are in a configuration that's only used for the drawing view. The threads are suppressed in the configurations used in the Assembly. I don't detail off-the-shelf hardware, so those files don't need threads at all.

[Frank_Oostendorp]

Keep in mind, export of BOM with thumbnails of multi config parts show all the same config in the picture. So all bolts show equal length.

[mp3-250]

In pdm the best would be a single configuration file, simple and effortless to maintain with the bugged tools sw offers.
even without pdm, if you have 100s of configurations it could not play nice to performance.

[Hansjoerg]

My current plan is to make parts with multiple configurations, and then save each configuration as a new part.

That's not a good idea! If you create your parts this way, the file size of the individual parts will be significantly larger than if you create them as individual parts. The more configurations the base part had, the larger the individual part will be.
Apparently, a few "corpses" of the configurations remain.


Toolbox:
I can only advise against using the toolbox (whether with configurations or as a single part).
1. toolbox parts are far too detailed (too many fillets)
2. they contain numerous equations
3. some of them contain undefined sketches.

Anyone who has ever taken part in a methodology and performance training course should keep their hands off the toolbox

[bnemec]

My current plan is to make parts with multiple configurations, and then save each configuration as a new part. If I need to fix something I can go back and do it from that one "template part" and save out the affected variants again, instead of having to go into each part and do the same.

Second what Hansjoerg says. Don't make all the configs and copy the file, it's a PITA to remove all the unwanted configs from the copied files. There's no way to copy a single config to new file.

Your concept is solid, just the implementation is a little off. Make one file then make sure to copy that when making new ones. Careful planning with this route will allow users to swap different hardware in assemblies and not break any mates or annotations on drawings. We colored the faces that are to be used for mates and never to be destroyed in the part model to help remind users of the goal.

[Hansjoerg]

Second what Hansjoerg says. Don't make all the configs and copy the file, it's a PITA to remove all the unwanted configs from the copied files. There's no way to copy a single config to new file.

Since SWX Version 2020 this is possible out of the box -> https://help.solidworks.com/2023/englis ... Redirect=1

Befor SWX 2020 it´s a job for a macro :-)

[martin]

That's not a good idea! If you create your parts this way, the file size of the individual parts will be significantly larger than if you create them as individual parts. The more configurations the base part had, the larger the individual part will be.
Apparently, a few "corpses" of the configurations remain.

Woah, thanks for letting me know, I will have to test that... I was also considering just exporting the configurations as parasolids and import them into new parts as dumb solids to minimize file size. But that means having to add mating references and assign properties afterwards for each one, so that process is perhaps more convoluted then just doing a bunch of "save as" on a single config part.

Since SWX Version 2020 this is possible out of the box -> https://help.solidworks.com/2023/englis ... Redirect=1

We are on 2023 and this is the method I was thinking of. But if SOLIDWORKS actually brings leftovers from the multi-config part over to the new parts then I would not do it this way.

[martin]

As a side note, the sample models from Cadbooster seem to make use of some clever entity naming, in addition to having a mate reference created for the same edge. I assume this is used by their Lightning add-in, but I wonder if this also helps to correctly reattach mates when using "Replace Components" if no mate references are present. I doesn't seem like this is present on any of the Toolbox components, so Toolbox probably just rely on mate references when a bolt type is being changed. Anyone here using entity naming for something useful or has some insight on this?

Edit: Documentation says face and edge names are used when replacing components https://help.solidworks.com/2023/englis ... operty.htm

[Pernils]

My current plan is to make parts with multiple configurations, and then save each configuration as a new part. If I need to fix something I can go back and do it from that one "template part" and save out the affected variants again, instead of having to go into each part and do the same.

Cadbooster's fastener models do look good. We require some additional ones, as well as we would need to configure custom properties for all of them. They do offer customization services for this which I am considering it. I'll probably do a trial on the lightning add-in to see how that works first, because it addresses one of my worries about having to browse through hundreds of files to find the right fastener.

The point about Toolbox licensing is valid, we have some professional and premium licenses, but a lot more standard licenses, so that could become a limitation.

Hmm

This is exactly the path SE have chosen. They call it "Family of parts".



(I haven't used it my self..)

[TTevolve]

I think this can differ depending on your MRP system. All of our standard bolts and screws are non-stock items, so I do what Glen said above, one part for each thread size, with configurations for each length. If I have a stock inventory item then it's 1 part file per part.

Same think would go for if you have PDM, then you almost have to 1 part file for each or you will have issues.

[mp3-250]

Hmm

This is exactly the path SE have chosen. They call it "Family of parts".



(I haven't used it my self..)

I think they took the concept from unigraphics-NX. it had family parts more than 20yrs ago

[mp3-250]

maintaining PDM data is already a pain with single configuration, not to mention that the file version upgrade utility is completely broken and iy is even more broken with multi configuration parts. the simpler yhe better.

[CarrieIves]

If you have multiple configurations in PDM, make sure to add a display data mark to each configuration. If you don't when the part has to be at a new configuration than the one it was saved at (For example you change from the 12mm L bolt to the 16mm L bolt) PDM thinks the part was modified. If it is a library part, I would expect users not to have the ability to check out and modify the library parts.

[JSculley]

Same think would go for if you have PDM, then you almost have to 1 part file for each or you will have issues.

Our hardware models are configured (via design table) and we've been using PDM since 2010. No issues. The part number, description, etc... are configuration specific properties. I have one socket head cap screw model that has hundreds of configurations and is used in thousands of assemblies.

When I'm adding hardware to an assembly, I just have to drag the model in once and from there it's just copying the same model over and over, changing the config when necessary.

[SolidKeke]

Absolutely you should use configurations. Someone said that library parts doesn't change, but their background data definately will change at some point and in that case you want to be able to maintain your files. You don't want to push changes to hundreds or thousands different part files, instead you open the design table, do the tricks and you're ready to go, all that in few minutes, instead of few days of error-prone work with separate files.

Another reason to use configurable files would be the ease of copying and modifying projects. Just few clicks and your library parts changed to a new size or length or whatever. No hazzle with replacing components and repairing mates/patterns that broke with your inconsistent separate library files.

I can't really say any good reason why to use separate files with library components and I probably can shoot down any reason someone else could possibly say

[AlexLachance]

We started with individual parts and then went with configurations instead, the reason being that we had a promoted assembly with each length in it and switching between configuration of the promoted assembly to reach the individual part would cause the drawing to lose it's references such as dimensions and balloons. That is not the case with configurations, though it forces you to adapt your working methods.

So, there are cases where we keep individual parts because the variations are not all that recurring and we just switch them manually when we need, so drawings will not lose links and there are cases where we have configurations instead because there are too many variations of the part and it varies too often in dimensions, so that when we switch the length of the part by changing configuration the drawing will not lose it's links.

So I'd say, it depends on the situation.

[jcapriotti]

Our hardware models are configured (via design table) and we've been using PDM since 2010. No issues. The part number, description, etc... are configuration specific properties. I have one socket head cap screw model that has hundreds of configurations and is used in thousands of assemblies.

When I'm adding hardware to an assembly, I just have to drag the model in once and from there it's just copying the same model over and over, changing the config when necessary.

Same here, our fastener library is all configurations since SolidWorks 98. We have over time split it some. Originally we just had "Hex Head Cap Screw.sldprt" with every size, thread, material, finish in one file. We know create a separate file for each material and finish so the configurations are just sizes and we can keep the configuration number down under 100 in most cases.

In our Windchill environment, our global team decided to make each a separate file when the library was built there. Now if you want a different size, you have to search and add it to the workspace, then go through the SolidWorks "replace" function. So much easier to just click and change the configuration.

[matt]

This is one area where Solid Edge is definitely a better tool. Solid Edge "Family of Parts" is like configurations, except all of the configs are separate files. You can manage them all from a single place. So you get the convenience of SW Configs with the stability of individual parts. In the end, it's a much better way to work. Plus, SE has great tools for swapping out parts in an assembly. SE FoP swaps are as easy as SW config swaps.

[jcapriotti]

Where used in PDM works pretty well, but not always. If you want to know the where used of a specific config in a file, you must first select the version of the file to select a specific config (standard part). Since the config file will likely get many versions as new parts/configs are added the where used will be across many versions, making the where used function in PDM worthless.

This appears to be fixed in 2023 (Maybe 2021). You can now select "All versions" and any configuration. Before, selecting "All versions" wouldn't let you select configurations.

[bnemec]

This appears to be fixed in 2023 (Maybe 2021). You can now select "All versions" and any configuration. Before, selecting "All versions" wouldn't let you select configurations.

image.png

This is good to know. However, the Configured Hardware ship has sailed from this port. But, we do still have some configurations that this might be helpful for. I think it should be a welcome enhancement.

[jcapriotti]

This is good to know. However, the Configured Hardware ship has sailed from this port. But, we do still have some configurations that this might be helpful for. I think it should be a welcome enhancement.

Sounds like a good candidate for a macro or custom program to easily allow swapping fastener models if going the non configuration route.

[Rob]

For what its worth I create a master file with configurations, but then I have a macro that rips out the individual parts.
Best of both worlds perhaps.

[DeanD]

Whether single part or a part with multiple configurations, there are a few settings keep in mind for performance.
Keep the image quality in the part file settings on the lower end for fasteners.
(i.e. McMaster Carr downloads are notorious for near max image quality and always hurts display and rebuild performance.)
For any threaded component, setup a derived configuration with threads suppressed.
Specific details can be shown with threads as needed, but generally showing threads is nothing but eye candy.
Once the desired configuration(s) are setup, lock all down with the "Feature Freeze" bar.
Can take a long while with a large quantity of configurations, but worth it to gain performance.
Hope this helps you choose a direction to best serve your needs.

[Dwight]

For any threaded component, setup a derived configuration with threads suppressed.

Better to leave off the threads in the main configuration.

[Glenn Schroeder]

Better to leave off the threads in the main configuration.

With only a few exceptions, the bolts in my parts library don't even have threads modeled. The one or two that do have them suppressed, and only showed the one time I needed to show them in a drawing (they're specialty bolts).

[SPerman]

I'm torn on this one. Pre-Solidworks the philosophy that was drilled into my head is 1 model = 1 part = 1 part number. As Matt mentioned above, NX handled this with part families. Solidworks has a different approach, and it appears to be fairly robust, but it still feels wrong from a philosophical point of view.

If I had it to do over today, I would probably adopt one model per thread style/dia/pitch, with lengths handled in the configuration. Going back and replacing all of the fasteners in my assemblies isn't going to happen, at least not without a 2nd engineer to help out.

Approach #2 would be individual parts, but the parts would all be derived from the same original model.

[DeanD]

Better to leave off the threads in the main configuration.

Thanks for ringing in on this and completely agree with you about that. But if the target audience/user base don't see the threads/features when the part is opened or inserted, confusion sets in. Yes, a training/instructing/experience issue, but in some long standing groups the approach is deemed incorrect.
Not many stop to sharpen their axe.